Using the Fillet Tool ( Fillet Feature ) - Part 2

PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2011/2012/2013

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook | LinkedIn

This is a continuation of the series of lessons for new Inventor Users. Check out this blog's table-of-content page for more topics in this series

TOPIC: USING THE FILLET TOOL - part 2

BEFORE YOU BEGIN

1. Download the dataset. The dataset files were created with Inventor 2011 to ensure compatibility with newer versions of Inventor.
2. Save it to a project folder of an existing Inventor project. Set the project active. Learn more about Inventor Projects and Project Files.
3. If there is any concept you do not understand, check out previous lesson: USING THE FILLET TOOL (FILLET FEATURE) - OVERVIEW.

INTRODUCTION

The Fillet tool can be used for creating various types of fillets/rounds. One of them is the constant-radius fillet. The constant-radius fillet applies only one radius at a time on any particular edge. To speed things up while creating fillets or rounds, we are going to learn how to use the All Fillets and All Rounds selection modes. The All Fillets mode allows you to select all interior edges on your part so that you can quickly apply fillets to them, while the All Round mode allows you to select all exterior edges on your part so that you can quickly apply rounds to them.


This lesson is a sequel to USING THE FILLET TOOL (FILLET FEATURE) - OVERVIEW. Endeavour to read it before continuing here.

OBJECTIVES

At the end of this lesson, the reader should be able to:

1. Describe and create a constant-radius edge fillet,
2. Describe and create an edge fillet using the All Fillets selection mode,
3. Describe and create an edge fillet using the All Round selection mode.

LOCATING THE FILLET TOOL

The Fillet tool could be found on:

1. RIBBON: Model tab > Modify panel > Fillet
   
   
2. SHORTCUT: F
   

procedures for creating a constant-radius fillet

In this section, we are going to learn how to create a constant-radius fillet.

1. Open the dataset file, constant_radius_fillet.ipt
2. Press F on your keyboard to launch the fillet tool. The Fillet dialog box is displayed (see Figure 3).
   
   
   
3. We are going to round all the edges on the top face of the part. On the Fillet dialog box > Constant tab and under Radius column, click 2mm. Type 20mm and press Enter. This sets 20mm as the new fillet radius.
4. Now click on all the edges on the top face of the part, one after the other. You model should resemble the Figure 5 below. The dialog box (see Figure 4) indicates that 6 edges have been selected.
   
   
   
   
5. Click OK to create the Fillet (see Figure 6).
   
   

ALTERNATIVE METHOD

This is an alternative and faster method to the one above.

1. Launch the Fillet tool.
2. On the Fillet dialog box, set the radius to 20mm.
3. On the right-hand side of the Fillet dialob box, set the Select Mode to "Loop."
4. Point at one of edges on the top face, and ensure that it highlights the top face. When the top face is highlighted, click.
5. Press OK to create the fillet.
   
   
   
   

REFERENCE

1. Autodesk Inventor 2010: Official Training Courseware.

I hope you learnt a lot from this lesson. If you have any questions, please drop a comment, and I will answer ASAP. Thank you.

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Using the Fillet Tool ( Fillet Feature ) - Overview

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PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2011/2012/2013

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook | LinkedIn

This is a continuation of the series of lessons for new Inventor Users. Check out this blog's table-of-content page for more topics in this series

TOPIC: USING THE FILLET TOOL (FILLET FEATURE) - OVERVIEW

BEFORE YOU BEGIN

1. If there is any concept you do not understand, check out previous lessons here.

INTRODUCTION

Fillets are smooth and round features commonly found on a edges of parts. Fillets are primarily used to reduce stresses on machine components/parts to reduce the potential of fatigue failure due to high stresses, and for aesthetic reasons. For the case of aesthetics, large filleted edges can be found on common household appliance e.g. coffee makers, reading lamps, hair dryers, phones, etc. These fillets help to improve handling experience (or ergonomics). So you can hold on to a phone without feeling acute pressure inside your palms because of the filleted edges of the phone.
The Fillet tool allows you to parametrically add a fillet feature to your part/component. This fillet could be a constant-radius fillet (where one radius is used to create the entire fillet) or a variable-radius fillet (where more than one radius is used to define the fillet along the edge). The Inventor Fillet tool offers an easy but powerful means of applying and modifying fillet features in your design.

OBJECTIVES

At the end of this lesson, the reader should be able to:

1. Describe the purposes of fillets on parts/components.
2. Explain the difference between fillets and rounds and give an example of how they are used.
3. Use the Fillet tool to create constant radius fillets.
4. State the guidelines for creating fillets.

LOCATING THE FILLET TOOL

The Fillet tool could be found on:

1. RIBBON: Model tab > Modify panel > Fillet
   
   
2. SHORTCUT: F

DEFINITION AND TYPES OF FILLETS

A fillet is defined by a single constant radius, or in the case of a variable fillet, by more than one radius. Technically, there are two types of fillets, namely, "Fillet" and "Round." The term "fillet" is used when a fillet is applied to an interior (or internal) corner/edge, (where the faces forming the corner/edge have an angle of 180 degrees or less between them). Fillets will also add material to your component/part. On the other hand, the term "round" is used when a fillet is applied to an exterior (or external) corner/edge. A round removes material from your component/part when created.
Figure 2 shows a part whose three (3) interior edges have been filleted, while Figure 3 shows a part whose exteior edges have been rounded. Note that both fillets and rounds are created with the Fillet tool.

CATEGORIES OF FILLETS

On the fillet dialog box, there are three important categories of fillets or rounds that can be created, namely:

1. Edge Fillet,
2. Face Fillet, and
3. Full-Round Fillet.

EDGE FILLET

As the name implies, an edge fillet is created along an edge of a part. An edge is formed by two adjacent faces, therefore, the Fillet tool will reshape the two shared face to create the desired fillet or round. Figure 4 shows a part with a single edge fillet.

FACE FILLET

A face fillet adds a fillet or round between two selected face sets, which need not share an edge. Figure 5 shows part with a face fillet applied between the top face and the left face.

full-round fillet

A full-round fillet adds a fillet or round that is tangent to three selected adjacent faces. The center face set is replaced by a variable-radius fillet. As can be seen in Figure 6, as full-round fillet is applied between the top, right, and bottom face of the part. The center (right) face is totally replaced with a fillet, which is tangent to all the three selected faces.

CONSTANT-RADIUS FILLET OPTIONS

The Constant Filet tab of the Fillet Dialog box contains the following creation methods and options.

	OPTION	DESCRIPTION
1.	Edge	Adds fillets or rounds to one or more edges of a part. All fillets and rounds created in a single operation become a single feature.
2.	Face	Adds fillets or rounds between two selected face sets. The face sets do not need to share an edge.
3.	Full Round	Adds fillets or rounds that are tangent to three adjacent faces. The center face is replaced by the fillet.
4.	Select Mode	Mode selection enables easy selection of objects to fillet. Select Edge, for edge selection priority, enables you to select individual edges on the part. So you have control of what edge to select Loop, for face selection priority, allows you to select all edges on a particular face in one click. Feature, for feature priority selection, allows you to select what feature to apply the fillet to. This works on parts with multiple features, so it gives your control over which feature to apply the fillet to, thereby ensuring that your do not select edges any other feature.
5.	Solids	This button is only available when multiple solid bodies exist in the part file. When this is the case, the user can click the solids button to select one or more solid bodies to use with the All Fillets and All Rounds selection options.
6.	All Fillets	Use the All Fillets check box to quickly select all fillet edges on the part. Select them both to have all edges on the part selected.
7.	All Rounds	Use the All Rounds check box to quickly select all round edges on the part. Select them both to have all edges on the part selected.

GUIDELINES FOR CREATING FILLETS

Although both fillets and chamfers are relatively simple shapes, they are often a challenge to create with consistency where multiple edges intersect. Following the guidelines presented here can improve your success in creating these features.

1. Avoid creating all of your fillets with a single feature. You will have a greater success creating and changing features with less edges selected.
2. Create these features on parallel edges of a part first. When you create additional features, you can select the resulting face to complete the remaining edges at the same time.
3. Pressing CTRL while clicking removes geometry from the selection.
4. Because fillets are considered finish features, consider creating them toward the end of the design process after all other features have been defined.
5. Avoid including fillets in your sketch geometry and instead create them as part features.

In the next two lessons, we are going to look at how to create constant-radius and variable-radius fillets, face fillets, and full-round fillets.

REFERENCE

1. Autodesk Inventor 2010: Official Training Courseware.

I hope you learnt a lot from this lesson. If you have any questions, please drop a comment, and I will answer ASAP. Thank you.

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Using the Sweep Tool (Swept Feature)

PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2011/2012/2013

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook | LinkedIn

This is a continuation of the series of lessons for new Inventor Users. Check out this blog's table-of-content page for more topics in this series

TOPIC: USING THE SWEEP TOOL (SWEPT FEATURE)

BEFORE YOU BEGIN

1. Download the dataset. The dataset files were created with Inventor 2011 to ensure compatibility with newer versions of Inventor.
2. Extract the content of the zip file using any unzipping utility.
3. Save the extracted file to a project folder of an existing Inventor project. Set the project active. Learn more about Inventor Projects and Project Files.
4. Go through the tutorial: Using and Understanding Work Planes in Autodesk Inventor. It will help you understand how to create work plane, which is important for creating with swept features.

INTRODUCTION

Swept features are one of the sketched features found in Autodesk Inventor. Swept features are created with the Sweep Tool. The term "sweep" in the context of swept features means extruding a sketch along a path, or curve. While the "Extrude Tool" sweeps along a straight line, the "Sweep Tool" sweeps the profile along the specified curve. The curve could be a straight line or any other complex two-dimensional or three-dimensional path. The Sweep tool requires two unconsumed and visible sketches in order to create a swept feature. One of the sketches must contain the profile to be swept (profile sketch), while the other sketch must contain the curve along which the profile will be swept (path sketch). The path sketch could be a 2D sketch or 3D sketch.

OBJECTIVES

At the end of this lesson, the reader should be able to:

1. Explain the concept of sweeping and swept features.
2. Use the Sweep tool for creating a Swept Feature.
3. Create a work plane that is parallel to an existing plane but coincident with a point along a path.

LOCATING THE SWEEP TOOL

The Sweep tool can be found on:

1. RIBBON: Model tab > Create panel > Sweep
   
   

CREATING A WORK PLANE FOR SWEPT PROFILES

One of the important techniques to be mastered when one is considering creating a swept feature is that of creating of work planes. Work planes are the basis for creating the profile and path sketches. You could start by creating the profile sketch first and the path sketch later, or vice versa. The choice is yours.

In this section, we are going to create a work plane and then create a path sketch on that work plane. The dataset file, using_sweep_tool_handle_3D_sketch.ipt, contains two 2D sketches containing 2D points which are used for creating a 3D sketch. We are going to create a work plane which is concident with the right endpoint of the 3D curve and parallel with th XZ plane (See Figure 2).

Let us now create the work plane.

CREATING THE WORK PLANE

1. Open using_sweep_tool_handle_3D_sketch.ipt.
2. Go the Model tab > Work Features panel > Plane. Click the flyout below Plane and select Parallel to Plane through Point (See Figure 3).
   
   
3. Expand the Origin folder and click on the XZ plane (See Figure 4). Next click the right endpoint (highlighted in Figure 2).
   
   
4. A new work plane is created.

Next we create a profile sketch on the newly-created work plane.

CREATING THE PROFILE SKETCH & THE SWEPT FEATURE

1. Right click on the newly-created work plane on the graphics window. Click New Sketch on the shortcut menu. A new sketch is created.
2. Refer to Figure 5. Click View Face on the Navigation Bar and click the name of new sketch (Sketch3 or Sketch4, depending) on the Model Browser.
3. Create two concentric circles with diameters 30mm and 26mm (as shown in Figure 5).
4. Click Finish Sketch and press "F6" on your keyboard.
5. Click Sweep on the Create panel (See Figure 1).
6. See Figure 7. Click the region between the two concentric circles as your profile. Next click the 3D curve as your path. Click OK to create the swept feature.
7. Right click the work plane (still visible on the graphics window) and click Visibility on the shortcut menu to turn off its visibility.
8. The completed model is shown in Figure 8.

I hope you learnt a lot from this lesson. If you have any questions, please drop a comment, and I will answer ASAP. Thank you.

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